HEIDENHAIN TNC 360 User Manual - Manual (Page 130)

6-7 TNC 360
6 Subprograms and Program Section Repeats
Program section repeat 2: machining from X=50 to
100 mm and Y=0 to 100 mm
Retract, reposition
Program section repeat 1: machining from
X=0 to 50 mm and Y=0 to 100 mm
100
–20,2
Y
X
Z
–30
–51
–70
11
50
89 100
21,646
78,354
R30
100
8
Y
X
Z
9
10
11
22
21
20
19
6.2 Program Section Repeats
Example for exercise: Milling with program section repeat without radius compensation
Machining sequence
• Upward milling direction
• Machine the area from X=0 to 50 mm
(program all X-coordinates with the tool
radius subtracted) and from Y=0 to
100 mm: LBL 1
• Machine the area from X=50 to
X=100 mm (program all X-coordinates with
the tool radius added) and from Y=0 to
100 mm: LBL 2
• After each upward pass, the tool is moved
by an increment of +2.5 mm in the Y-axis.
The illustration to the right shows the block
numbers containing the end points of the
corresponding contour elements.
Part Program:
0 BEGIN PGM 360067 MM
1 BLK FORM 0.1 Z X+0 Y+0 Z–70
2 BLK FORM 0.2 X+100 Y+100 Z+0 ..................... Note: the blank form has changed
3 TOOL DEF 1 L+0 R+10
4 TOOL CALL 1 Z S1000
5 L X–20 Y–1 R0 FMAX M3
6 LBL 1
7 L Z–51 FMAX
8 L X+1 F100
9 L X+11.646 Z–20.2
10 CT X+40 Z+0
11 L X+41
12 L Z+10 FMAX
13 L X–20 IY+2.5
14 CALL LBL 1 REP40/40
15 L Z+20 FMAX
16 L X+120 Y–1
17 LBL2
18 L Z–51 FMAX
19 L X+99 F100
20 L X+88.354 Z–20.2
21 CT X+60 Z+0
22 L X+59
23 L Z+10 FMAX
24 L X+120 IY+2.5
25 CALL LBL 2 REP40/40
26 L Z+100 FMAX M2
27 END PGM 360067 MM